[SI-LIST] 答复: Re: Does power/ground pair edege radiation noise really matter in the EMI test?

  • From: Xu Shuai <xushuai@xxxxxxxxxxxxxxxxxx>
  • To: 'LIU Luping' <liuluping@xxxxxxxxxx>, 'Jory McKinley' <jory_mckinley@xxxxxxxxx>, 'Lee Ritchey' <leeritchey@xxxxxxxxxxxxx>, 'steve weir' <weirsi@xxxxxxxxxx>
  • Date: Tue, 28 Dec 2010 14:22:27 +0800

Hi Luping and all,
I do not think a 4mil core power/ground pair can produce very strong
radiation, maybe the radiation has been dominated by other parts, such as
other power planes, the cables, the backplane connectors,etc. To my
experience it is not easy to draw general EMC conclusions from a complex
system. There are too many related factors.

We have design many simple test PCBs include microstrip and stripline types
and there are also some decaps and clock nets on them. We simulated and
measured the farfield radiation. The results matched very well(<4dB).

Stitching GDN via is effective to reduce the radiation from the edge, but if
there is other dominant radiation you will not find the impact of these
stitching vias.

I am doubt that the stitching via could impact the resonance characteristics
too much because to a thin PCB structure usually the radiation loss is very
small compared to the dielectric and conduct loss. So the difference is just
the open and short boundary conditions. They do not have great difference
except resonance frequency.

Best regards,
Shuai

-----邮件原件-----
发件人: si-list-bounce@xxxxxxxxxxxxx [mailto:si-list-bounce@xxxxxxxxxxxxx]
代表 LIU Luping
发送时间: 2010年12月28日 12:11
收件人: Jory McKinley; Lee Ritchey; steve weir
抄送: Istvan Novak; si-list@xxxxxxxxxxxxx
主题: [SI-LIST] Re: Does power/ground pair edege radiation noise really
matter in the EMI test?

Dear all:
    Sorry for mistake operation and much appriciate for your replies.
Shall we conclude that the answer to this question is YES, although still
some puzzles:
    As Istvan and Brad replied,we can separate this problem into two case:

 1) Power plane on the outside of the board stackup,e.g. microstrip type,may
be treated as 
Patch antenna and expect to radiate bit more energy than the striplines
mode(case 2),but the 
noise source seens not directly from the eedge radiation,as Lee Ritchey
recommand:

Pantic-Tanner, De. Zorika etal, "Radiation Edge Effects in PCBs, (20H rule),
San Francisco State University, May 2000.

   We have a test digital board with power/ground pair (4mil core) on the
2/3 layer of a 8 layers board, all decouple capacitor
mount on the top side with few hundreds mils distance from the power pin of
the chip,have similar PI performance with a 
compare board which the power/ground pair in side the stackup and the decap
mount on the bottom side,but the RE test shows 
5~10dB difference from hundreds to 3GHz,include the 375 MHz and higher.

   Should we pay attention to the edge noise here? it seens nothing to do
with this noise source,stich GND via is not effective now.

  
2)Power plane inter side of the board stackup,e.g.stripline type. many
comments here,especially on the excite souce(signal line/via/SSN,etc.),
  the coupling path, and the edge radiation mechanism,all have different
views,and the solution,.
  
  From the excite souce,the parasitic inductance of via will consist an
natural filter that isolate most of these noise into the plane. 
  Due to the presence of  via and trace,prediction of edge radiation levels
using antenna models rarely produces accurate results.
  
  As for the solution,stich GND via may be not so perfect,one of the reason
is the edge connector,then not all four sides can be grounded,
and it need two GND plane at top and bottom side; another reason is that the
reflections from the edges reflect back into the PCB, increasing 
the magnitude of internal resonant peaks and secondary coupling backonto
traces and vias. The coupling can be significant enough to create
signal integrity problems such as ground bounce and simultaneous switching
output (SSO) noise.

  Am I right?

Best Regards, 
LIU Luping 
***************************************************************** 
   This e-mail and its attachments contain confidential information from
HUAWEI, which is intended only for the person 
or entity whose address is listed above. Any use of the information
contained herein in any way (including, but not 
limited to, total or partial disclosure, reproduction, or dissemination) by
persons other than the intended recipient(s) 
is prohibited. If you receive this e-mail in error, please notify the sender
by phone or email immediately and delete it! 
***********************************************
----- Original Message ----- 
  From: Jory McKinley 
  To: Lee Ritchey ; steve weir 
  Cc: Istvan Novak ; liuluping 41830 ; si-list@xxxxxxxxxxxxx 
  Sent: Tuesday, December 28, 2010 6:10 AM
  Subject: Re: [SI-LIST] Re: Does power/ground pair edege radiation noise
really matter in the EMI test?


  Hello Lee,
  We have a case in which an existing customer design was not functioning
due to one direct path to path coupling in the PLL.  This path to path
coupling was one resonate structure path (resonate at critical PLL
frequency) to the PLL power path.  We came in and found the amount of
coupling was in the -20dB range which based on PLL simulations should have
been less than -50dB at this critical frequency.  We caught this path on the
old package (plus some others not related in separate blocks ) and spun a
new package with coupling below the -50dB target.  The re-spun package is
fully functional to date and trying to get customer permission to turn into
a paper.  
  There are other cases and admittedly more the common as you point out in
which it is less clear as to what the exact coupling path that has created
issues with a product.  For example, we are working on which shows at least
5 coupling paths that are individually close to the allowable coupling but
collectively sum above the absolute maximum coupling.  Of these paths one of
them has a resonate in the frequency of interest which to be safe we took
care to damp this path while trying to further isolate the others. 

  Regards,
  -Jory


------------------------------------------------------------------
To unsubscribe from si-list:
si-list-request@xxxxxxxxxxxxx with 'unsubscribe' in the Subject field

or to administer your membership from a web page, go to:
//www.freelists.org/webpage/si-list

For help:
si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field


List technical documents are available at:
                http://www.si-list.net

List archives are viewable at:     
                //www.freelists.org/archives/si-list
 
Old (prior to June 6, 2001) list archives are viewable at:
                http://www.qsl.net/wb6tpu
  



------------------------------------------------------------------
To unsubscribe from si-list:
si-list-request@xxxxxxxxxxxxx with 'unsubscribe' in the Subject field

or to administer your membership from a web page, go to:
//www.freelists.org/webpage/si-list

For help:
si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field


List technical documents are available at:
                http://www.si-list.net

List archives are viewable at:     
                //www.freelists.org/archives/si-list
 
Old (prior to June 6, 2001) list archives are viewable at:
                http://www.qsl.net/wb6tpu
  

Other related posts: